Contents of a Solid
Functions Introduced:
• ProSolidFeatVisit()
• ProSolidQuiltVisit()
• ProSolidAxisVisit()
• ProSolidCsysVisit()
• ProSolidFeatstatusGet()
• ProSolidFeatstatusSet()
• ProSolidFeatstatusWithoptionsSet()
• ProSolidFeatstatusflagsGet()
• ProSolidFailedFeatsList()
• ProSolidFailedfeaturesList()
• ProSldsurfaceShellsAndVoidsFind()
• ProSolidToleranceStandardGet()
• ProSolidToleranceStandardSet()
• ProSolidToleranceStandardVersionSet()
• ProSolidToleranceStandardVersionGet()
• ProSolidToleranceStandardUpdate()
The following visit functions enable you to access the various types of objects inside a part or assembly:
• ProSolidFeatVisit()—Visits all the features, including those used internally (which are not visible to the user). You can also use this function to visit the components of an assembly.
• ProSolidSurfaceVisit()— Visits the surfaces of the model only if the model has a single body else returns the error PRO_TK_MULTIBODY_UNSUPPORTED. This includes all surfaces created by solid features, but not datum surfaces.
• ProSolidQuiltVisit()—Visits all the quilts in a part or an assembly.
• ProSolidAxisVisit()—Visits all the axes in a part or an assembly.
• ProSolidCsysVisit()—Visits all the coordinate system datums in a part or an assembly.
The function ProSolidFeatstatusGet() retrieves a list of the integer identifiers and statuses of all the features in a specified solid in the order in which they are regenerated. The integer identifier of a feature is the value of the id field in the ProFeature object and also the INTERNAL ID seen in .
The function ProSolidFeatstatusSet() enables you to set the regeneration order and statuses of the features in the solid.
The function
ProSolidFeatstatusWithoptionsSet() assigns the regeneration order and status bit flags for the specified features in a solid based on the bitmask containing one or more regeneration control bit flags of the type
PRO_REGEN_* defined in
ProSolid.h. Refer to the
Regenerating a Solid section for more information on the bit flags.
The function
ProSolidFeatstatusflagsGet() retrieves the array of integer identifiers of the features in a specified solid and the corresponding array of bitmasks representing one or more feature status bit flags of the type
PRO_FEAT_STAT_* defined in
ProFeature.h. Refer to the
Core: Features section for more information on the feature status bit flags.
The function ProSolidFailedFeatsList() retrieves the list of identifiers of failed features in a specified solid.
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Note:
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From Pro/ENGINEER Wildfire 5.0 onward, the function ProSolidFailedFeatsList() has been deprecated. Use the function ProSolidFailedfeaturesList() instead. Pass NULL for the input arguments co_failed_ids and co_x_failed_ids while using ProSolidFailedfeaturesList() in the Resolve mode.
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The function ProSolidFailedfeaturesList() retrieves the list of identifiers of all or any of the failed features, children of failed features, children of external failed features, or both the features and their children.
The function ProSldsurfaceShellsAndVoidsFind() returns an ordered list of surface-contour pairs for each shell and void in a solid.
The surface-contour pairs describe the shell faces and are specified by the ProSldsurfaceShellface objects. If the contour field in the ProSldsurfaceShellface object is NULL, it means all the contours in the geometry belong to the same surface and the shell_faces array contains only one surface ID. However, if the contours belong to different shells, the shell_faces array contains items equal to the number of contours.
The ordered list of surface-contour pairs is specified by the ProSldsurfaceShellorder objects; each of this object contains the following fields:
• orientation—Specifies the shell orientation. If this field is 1, the shell is oriented outward, if it is -1, the shell is inward oriented meaning it is a void.
• first_face—Specifies the index in the array of ProSldsurfaceShellface objects.
• number_of_faces—Specifies the total number of shell faces.
• ambient_shell—Specifies the index in the array of ProSldsurfaceShellorder objects.
The function ProSolidToleranceStandardGet() returns the tolerance standard assigned to a solid. Use the method ProSolidToleranceStandardSet() to set the tolerance standard for a solid. After you set the tolerance standard for a solid, you must regenerate the solid, if required. The function does not regenerate the solid.
The function ProSolidToleranceStandardVersionSet() sets the version for assigned tolerance standard of a specified solid.
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Note:
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In the user interface, this operation asks to regenerate the solid. The function ProSolidToleranceStandardVersionSet() does not perform regeneration itself.
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Use the function ProSolidToleranceStandardVersionGet() to get the version for assigned tolerance standard of a specified solid.
Use the function ProSolidToleranceStandardUpdate() to update the solid to the most current version of its tolerance standard. The function does not regenerate the solid.